CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

HELPAn engineering application of OF

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 2, 2005, 06:15
Default There is an engineering proble
  #1
Member
 
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 7
leosding is on a distinguished road
There is an engineering problem which need CFD to analyse.
The hot flue with fine dust flows into a mix chamber and is quenched by the fresh air blowered into the chamber. The mix effect,( the uniformity of temperature at chamber outlet) is critical.
Now I want to analyse it with OF, but I can not find a proper standard solver for it.
Who can give me some hints for it, which standard solver may be modified to meet my case.
I think these models are need:
turbulence model, heat transfer of gas and particle (maybe dig it out form spray model?).

Thanks a lots in advance!
leosding is offline   Reply With Quote

Old   December 2, 2005, 06:26
Default dieselFoam can do this. The
  #2
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 692
Rep Power: 18
niklas will become famous soon enough
dieselFoam can do this.

The only thing you might need to do is to implement
the properties of your particles.

N
niklas is offline   Reply With Quote

Old   December 2, 2005, 08:30
Default Niklas, Thanks! When I compl
  #3
Member
 
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 7
leosding is on a distinguished road
Niklas,
Thanks!
When I complete it, the result picture will be posted here. It will be my first industry application of OpenFOAM.
leosding is offline   Reply With Quote

Old   December 3, 2005, 09:50
Default Hi Niklas, I fight with diese
  #4
Member
 
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 7
leosding is on a distinguished road
Hi Niklas,
I fight with dieselFoam whole day, but I have no idea for it.
My case(one industry equipment, so big; it has been done with commercial CFD software.) is that there are two inlets, one for fresh air, another one for hot flue carried dust, no reaction, is steady flow.
I don't know where to change for particle with diameter, density, specific heat as you pointed out.
Would you (or some experienced people) give me more detailed?
leosding is offline   Reply With Quote

Old   December 8, 2005, 00:29
Default Hi FOAMers, Would someone pro
  #5
Member
 
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 7
leosding is on a distinguished road
Hi FOAMers,
Would someone provide one basic lagrange model application solver?
In Hrv's MFIX training material(in their wiki) there is a tutorial, but I cannot find it in openfoam release.

thanks a lots.
leosding is offline   Reply With Quote

Old   December 8, 2005, 14:29
Default That would be because it has n
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,741
Rep Power: 20
hjasak will become famous soon enough
That would be because it has not been released - it's basically a simple solver for massless particles carried by the incompressible transient flow solution (built into icoFoam). I am a bit anxious of just passing it over because I haev done a number of lagrangian-related bug fixes and until that makes it into the release I cannot guarantee that the thing will work "out-of-box".

However, if you feel adventureous and don't mind getting your hands dirty, I have no objections in passing it over in the current state.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   December 8, 2005, 21:26
Default Thanks for your kindness. I w
  #7
Member
 
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 7
leosding is on a distinguished road
Thanks for your kindness.
I wanna fight with it based on your current works for lagrangian solver if you could post it here.
leosding is offline   Reply With Quote

Old   December 9, 2005, 06:54
Default for starters, get the case ru
  #8
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 692
Rep Power: 18
niklas will become famous soon enough
for starters,
get the case running without particles.
THEN try to use a standard liquid to get the case properly set up, for instance water.
Turn off evaporation (in sprayProperties).
That way you will only have energy exchange between particles and gas and no mass transfer.

and you specify initial droplet/particle condition in injectorProperties and sprayProperties (atomizationModel)

You obviously also need to turn off the breakupModel.

Once that is workin you can start modifying the liquid (solid) properties by adding a new liquid
(src/thermophysicalModels/liquids)

N
niklas is offline   Reply With Quote

Old   June 11, 2008, 07:16
Default Hi FOAMers, Sorry for digg
  #9
Member
 
lord_kossity's Avatar
 
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 7
lord_kossity is on a distinguished road
Hi FOAMers,

Sorry for digging out this old thread, but it's a 100% relating to what I'm trying to achieve.

My goal is to add some new liquids, but when I look up the .H files of the different already implemented models, I'm confused about the different numbers stated in brackets e.g.

liquid(18.015, 647.13, 2.2055e+7, 0.05595, 0.229, 273.16, 6.113e+2, 373.15, 6.1709e-30, 0.3449, 4.7813e+4).

What do the numbers stand for?

Thanks for any help,
Andreas
lord_kossity is offline   Reply With Quote

Old   June 11, 2008, 08:03
Default The doxygen docs for 'liquid'
  #10
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 774
Rep Power: 17
olesen will become famous soon enough
The doxygen docs for 'liquid' or the corresponding header
src/thermophysicalModels/liquids/liquid/liquid.H
should help you.

There are member functions corresponding to each of the constructor parameters too.
olesen is offline   Reply With Quote

Old   June 11, 2008, 09:04
Default Thank you! Now it's clear w
  #11
Member
 
lord_kossity's Avatar
 
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 7
lord_kossity is on a distinguished road
Thank you!

Now it's clear what the numbers in the liquid line mean.

It is also clear that rho_, pv_, etc. refer to the NSRDS functions.
And now it is getting unclear again. What do the scalars in the different NSRDS functions stand for?
lord_kossity is offline   Reply With Quote

Old   June 11, 2008, 10:50
Default OK, OK, obviously these are
  #12
Member
 
lord_kossity's Avatar
 
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 7
lord_kossity is on a distinguished road
OK, OK,

obviously these are coefficients for some interpolation functions, aren't they?

Can you please give me a reference, where I can look them up?

Thanks in advance,
Andreas
lord_kossity is offline   Reply With Quote

Old   June 12, 2008, 10:19
Default Assuming you havent been able
  #13
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 692
Rep Power: 18
niklas will become famous soon enough
Assuming you havent been able to execute the command
find $FOAM_SRC -name "NSRDS*"
I suggest you start here
OpenFOAM/OpenFOAM-1.4.1/src/thermophysicalModels/thermophysicalFunctions/NSRDSfu nctions
niklas is offline   Reply With Quote

Old   June 12, 2008, 10:54
Default To find the NSRDS functions wa
  #14
Member
 
lord_kossity's Avatar
 
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 7
lord_kossity is on a distinguished road
To find the NSRDS functions wasn't the problem.

"them" related to the coefficients themselves. where can I find them? Am I too dumb to see their description in the NSRDSfunction directories?
lord_kossity is offline   Reply With Quote

Old   June 13, 2008, 01:58
Default from... NSRDSfunc0.H
  #15
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 692
Rep Power: 18
niklas will become famous soon enough
from...
NSRDSfunc0.H
scalar f(scalar, scalar T) const
{
return ((((f_*T + e_)*T + d_)*T + c_)*T + b_)*T + a_;
}

NSRDSfunc1.H
scalar f(scalar, scalar T) const
{
return exp(a_ + b_/T + c_*log(T) + d_*pow(T, e_));
}

NSRDSfunc2.H
scalar f(scalar, scalar T) const
{
return a_*pow(T, b_)/(1.0 + c_/T + d_/sqr(T));
}

NSRDSfunc3.H
scalar f(scalar, scalar T) const
{
return a_ + b_*exp(-c_/pow(T, d_));
}



etc...
niklas is offline   Reply With Quote

Old   June 13, 2008, 02:40
Default Yeah, but which values do I se
  #16
Member
 
lord_kossity's Avatar
 
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 7
lord_kossity is on a distinguished road
Yeah, but which values do I set for a, b, c, ...?
lord_kossity is offline   Reply With Quote

Old   June 13, 2008, 03:36
Default lets look at C7H16.H vapor
  #17
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 692
Rep Power: 18
niklas will become famous soon enough
lets look at C7H16.H

vapor pressure is declared as
NSRDSfunc1 pv_;

and in the constructor we have

pv_(87.829, -6996.4, -9.8802, 7.2099e-06, 2),

and the constructor for NSRDSfunc1 is
NSRDSfunc1(scalar a, scalar b, scalar c, scalar d, scalar e)

i.e. a=87.829, b=-6996.4, etc...
niklas is offline   Reply With Quote

Old   June 13, 2008, 04:14
Default aha, well thats from the .H he
  #18
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 692
Rep Power: 18
niklas will become famous soon enough
aha, well thats from the .H headers

Source:
NSRDS - AICHE
Data Compilation Tables
of Properties of
Pure Compounds

Design Institute for Physical Property Data
American Institute of Chemical Engineers
345 East 47th Street
New York, New York 10017

National Standard Reference Data System
American Institute of Chemical Engineers

T.E. Daubert - R.P. Danner

Department of Chemical Engineering
The Pennsylvania State University
University Park, PA 16802
niklas is offline   Reply With Quote

Old   June 13, 2008, 04:42
Default Well, yesterday I googled for
  #19
Member
 
lord_kossity's Avatar
 
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 7
lord_kossity is on a distinguished road
Well, yesterday I googled for some of these key words but I did not find any tables.

Don't you have any other references, preferably some books?

btw, thanks for the patient iteration of the question!
lord_kossity is offline   Reply With Quote

Old   June 13, 2008, 04:45
Default those are books, I think 7 of
  #20
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 692
Rep Power: 18
niklas will become famous soon enough
those are books, I think 7 of them,
thick like @$"! and just full of tables.

what liquid are you interested in?
niklas is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
y+ application vivek.k.yakkundi FLUENT 2 October 22, 2007 12:17
Which application to use ploceus OpenFOAM Running, Solving & CFD 1 December 7, 2005 19:41
MPI Application in HPC wendy CD-adapco 0 May 19, 2005 01:50
application of cfd samuel R devadoss Main CFD Forum 0 March 15, 2004 04:38


All times are GMT -4. The time now is 14:10.